Extruded bar

This command positions the extruded bars in the assembly.

Creation stages / Use:

Select Modeling > Extruded Bar... command from the drop-down menu.

To be able to use the extruded bars, it is essential that the libraries required for the project be referenced beforehand. The referencing is done via the Add reference contextual command from the references icon in the project tree.

Select a type of extruded bar in the drop down list.
Select the code of the extruded bar in the drop down list.

This command allows you to position an extruded bar on each selected edge, segment, profile or face.

Select the reference profile, a segment, edge or face.
Select the reference direction to be able to orient the extruded bar.

This command positions the extruded bar by selecting its 2 end points.

Select the first and second point.
Select the reference direction to be able to orient the extruded bar.

This command positions the extruded bar on a frame and indicates its length.

Select the destination frame.
Enter the length of the extruded bar.

This command allows to position the extruded bar by constraint positioning.

Enter the length of the extruded bar.
Position the extruded bar in the graphic area (if the dialog is unpinned, you are able to constraint your extruded bar).

This command allows to position the extruded bar on a segment and generates a section view by automatic box as well as a zoom on it.

Select the destination segment.

This option facilitates installation on large structures by calculating a cut box based on the length of the selected segment and the section of the selected extruded bar, and places the cut box frame where the user has clicked on the segment.
Cross section is automatically activated as well as the zoom on it (normal to the XY plane of the box cut at the user's click location).
See the Positioning help paragraph below for further explanations.

Enter the orientation of the extruded bar. The orientation is a rotation around the longitudinal axis.
Check or uncheck the Reverse extruded bar. This option reverses the direction of the extruded bar.
Select the offset type by clicking one point in the extruded bar preview of the dialog. The selected point becomes blue. The longitudinal axis of the extruded bar will be on this point. It can also be changed by double-clicking one of the yellow points (in the graphic area)
If required, enter the value of the horizontal offset.
Select the type of vertical offset from the drop down list.
If required, enter the value of the vertical offset.

Positioning help:

	Three icons in the top right-hand corner of the graphics area can be used to facilitate profile positioning (features available for all installation modes except the constraint installation mode). The graphic cut is ephemeral, which means that if the user changes positioning mode, or if the user quits the extruded bar dialog, then the cut view is deleted and the initial graphic configuration is restored.
	Edit cut by box: The ephemeral cut box dialog opens, allowing you to configure it (dimensions, color, etc.). Ephemeral box cuts are always initialized with values that ensure the box to be centered and of a size close to that of the installed extruded bar.
	Cut by box: This icon allows to activate/deactivate the previously created cut.
	Focus on section: This icon allows to modify the graphic view to be focus on the cut section (normal to the XY plane of the cut by box).

The orientation can be done in the graphic area by dragging handles.
The offset can be modified by double-clicking one point in the dialog preview.
If a face is selected with the first option, an extruded bar will be positioned on each edge of this face. It is the same thing for the profile, an extruded bar will be positioned on each line of this profile.
The extruded bar command is also available by contextual menu from a sketch.

The case of a family of an extruded bar assembly with boolean drivers to manage inclusions into the generic is not managed. In place parts of the generic assembly must not have conditions to activate/deactivate them.

To use the same profile than an existing one, just select it before using the Extruded bar command.
While the definition of the extruded bar generic document, it is possible to set Possible values to the length parameter used by the extruded bar. This avoids to create instances with length 100m. TopSolid uses the first possible value just above the true length. For example, including an extruded bar on a profile of 2,5m, if 1m, 3m and 10m have been defined as possible values in the generic document, the created instance will use the length 3m. This is quite interesting when the generic document contains a multitude of operations because the computation time during the inclusion is considerably optimized.

Advanced Options:

Substituable in upper levels:

This option allows to authorize the substitution (replacing) of the extruded bar when the assembly document is included into another assembly.

When it is not checked, the extruded bar will be greyed in the substitution dialog box.

See the sub-component substitution command for more details.

Part creation method:

This menu allows you to choose to create a derived part or a local part. The default mode can be set in Tools > Options > Assembly > Extruded Bars > Part creation method.
The template document used for derived extruded bars will also be used for local parts.
Working in a local part brings a considerable gain in performance (opening/closing of documents, refreshing, saving, checking-in, adding extruded bar, importing/exporting packages, TopSolid file size, package size, ...).
Please note that some operations are incompatible with the local parts:

Transformation
Mirror creation

Profile decomposition:

This menu allows you to choose how to decompose an extruded bar when placing it on a profile:

No: 1 set of tangent segments = 1 extruded bar.
Partial: 1 set of tangent segments = 1 extruded bar except for collinear straight segments.
Yes: 1 segment = 1 extruded bar.

The horizontal profile is composed of 2 segments

Modifications / Additional information:

To modify the type of extruded bar, its offset, its orientation, use the Edit contextual command.
The extruded bar family can contain drivers to be able to modify them during extruded bar inclusion.
An extruded bar can be an assembly to allow to manage a different material for each part of the assembly as for example a extruded bar with a seal.
During the in place edition of an extruded bar, it is possible to associatively hang on the assembly.
The Replace contextual command allows to interchange several extruded bars at the same time.

Operations on extruded bar:

When an extruded bar has operations other than miter trim, main trim or planar trim, it is identified by a specific management operation in Analysis stage with a parameter Operated = True in Parameters > System Parameters folder of the Entities tree. This parameter can then be retrieved in a bill of material, allowing the user to make a more detailed drafting of these extruded bars.

Curved extruded bar:

Extruded bar components can be included on 2D or 3D sketch with splines or arcs.

Into a sketch, tangent curves will create a single curved extruded bar.

Extruded of extruded bars:

In an assembly document, it is possible to included several extruded bars and to provide the Extruded bar function document in order to define an extruded bar of extruded bars. This allows for example to create an extruded bar with its seal. This extruded bar behaves like any part extruded bar and supports cutting operations (miter trim, main trim, curved extruded bar, ...).


	Example of extruded bar made of 2 extruded bars.